I am having a problem with the router engaging the material after having set the Z Axis to zero. The machine runs fine , goes home, goes to zero, goes through the motion of the router running the part but I cannot get it to raise or lower beyond the Z zero setting. Checked the wires even replaced the wiring with new wiring to the Z Axis motor. I even recalibrated the Z Axis distance thinking it might be that. That did not help either. The only place I can think it might be is in the Glbr sequence. Been trying to fix the problem for about 3 days now. Ran out of ideas, thought maybe you guys may be able to enlighten me.
What cam software are you using? Do post your g-code file so we can look at it. Also, what controller are you using? - if a grbl one post your grbl settings. Alex.
I am not a computer whiz been trying to figure out how to send info to you, best i come up with is shift print screen?
When you are typing a message, use the 'upload a file' button at bottom right to attach a fie, either text or picture. You can also drag and drop pictures onto the message.
thankyou. That is code generated for a laser cutter Code: ; GCODE Generated bY- cam.openbuilds.com on 2025-03-24 G21 ; mm-mode ; Created bY- OpenBuilds CAM G54; Work Coordinates G21; mm-mode G90; Absolute Positioning M4; DY-namic Power Laser On M4; DY-namic Power Laser On is only used for laser cutters. then a few lines later is tells it to go to Z0, which is just in contact with the surface of the material, and then it goes below that by only 0.094mm, not really far enough to be seen. If you have enabled 'soft limits' then turn it off now. Go into CAM and remove the existing toolpaths and replace them with milling paths rather than laser cuts, regenerate the Gcode. Let's just be clear on the correct sequence for running a job (besides choosing milling operations in CAM, rather than laser) 1 - power up the machine 2 - power up the computer and start OpenBuildsCONTROL 3 - click the 'Home All' button so that the machine can find home , everything needs a sense of home Home, Fusion360 and G53 Z moves 4 - load the Gcode file 5 - jog to the material 0,0,0 point and click the relevant setZero buttons to teach the machine where 0 is for this part, this must match whatever was used in the CAM for the origin 6 - jog Z up a little and start the router (unless the controller can turn it on via Gcode) 7 - click 'Run Job' button with soft limits off and a proper home sequence, and also the correct Gcode, all should be well, but if it is not, we will need details...
I have used both M3 and M4 for the code does not change laser nor router operation. The machine is zero for home works great, even set the z operation and it goes above the part x,y, function works the z command does not engage to cut the part out. I use the cam program and select the operation for CNC no options it generates the code. The router is manual switch operated. I will reset the GrblHal code on the soft limit see if it effects the Z operation. G54; Work Coordinate. Is on the machine selection setting, mine is a workbee 1510 with no other info following G54.
Nope no change. My question is why the program does not see and obey the Z command. It sees the X, Y, commands but not the Z settings.
These are your Z commands - none of the commands in your g-code file go any lower than this, and your Z safe move is only to Z0 - presumably to the surface of the material if that is where you set Z zero. You are in mm mode, so your maximum (only) plunge is 0.094 of a mm. I'm pretty sure this is a cad/cam problem, so please talk us through how you created the g-code file - what software you used etc. Alex. PS, I believe @David the swarfer was saying that the M4 line was an indication that the g-code file was created for a laser, not that M4 was the whole problem.
Software is openbuilds, my machine is a work bee 1510, Cam: open drawing: Select All: Create Toolpath: (For some reason it flashes unknown error Lasstused then goes away) Configure Toolpath: Select Operation: CNC Vector (No Offset) The settings are: Endmill/Pen Diameter 3.12 mm: Z Safe Height 0 mm; Spindle RPM 1000 rpm: Cut Depth 3 mm: Cut Depth per Pass 3 mm: Feed Rate (X/Y) 150 mm/min: Feed Rate Plunge -0.1 mm/min. Advance Settings: (Which I don't change): Cutting Direction: Climb: Geometry Merge No: Plunge: Ramp in (beta) Experimental No: Cut Depth Start 0 mm: Tabs Height 6 mm Tabs Spacing 50 mm; Select Apply and Preview Toolpath Generate G-Code Save G-Code (save goes to download file) Open File Set the zero to part and change the X Y to the direction -X -Y and the depth setting That's it.
NB NB NB DONT DO THIS BEFORE PROVIDING REVIEWS, AS CLEARING LOCAL STORAGE WILL ALSO REMOVE ANY INCORRECT VALUES YOU HAVE IN TOOLPATH SETTINGS. JUST PROVIDING THIS INFO IF AFTERWARDS YOU WANT TO FIX LASTUSED ERROR Click Factory Reset to clear corrupted LastUsed from your browser's localstorage ------ Not what the gcode you uploaded reflects. Provide screenshots or even better Project Export rather than typing out what you have We can import the saved project and check what you have set, so best way to review.
On the G-Code 3mm setting I tried entering my depth number -0.094 it did not like it. It likes the whole number -1.000 or greater. ?? don't know why it won't except -0.000 entries.
Negative Depth? - how do you propose it will ADD material? Enter positive numbers. I want to cut "3mm" deep after all (not I want to Cut negative 3mm deep) Also, thats very very little distance, you won't see a 0.1mm move with the naked eye Average depth per pass is around 1/2 the endmill's diameter, doubt thats a 0.2mm endmill? What is the plan there
The material I cut is 1/8 thick the -0.094 setting is the final depth just before the getting into table. if I place the negative number into Cam final depth cut, it does not compile the job, so that is why I left it set at 3 mm in Cam. Hope this makes sense. I added the work file, the X, Y, Z depth and S settings are not edited.
Positive speed for plunge as well please, can't move at negative speeds yet, time travel still not invented. Plus, think what you are typing. 0.1mm in per minute! - no man you can't move that slow... Correct it won't compile... you want to do a through cut of material? Its 1/8 inch = 3.175mm (for Final Cut Depth)... at some depth per pass (+-1/2 of 1/8" endmill, somewhere like 1.5-1.8mm depth per pass will do - call it 1.8mm per pass will do for woods, acrylics etc) Other issues: - missing Z safe height... got to lift that tool between cuts - feedrate insanely low - use proper feedrates - stop trying to use negative numbers - no offset is probably wrong too, looking at the CAD file I would have suspected inside cut for the holes and outside cut for the profile. Should be more like that (feedrate thumbsucked, not sure what material you have - refer speeds and feeds charts)
I do have a question regarding this machine. Do you think I could cut 3/4 thick aluminum material with it. Thought about getting a heavier milling machine but if this machine is capable i will use it.
Yes, a workbee is capable of cutting 3/4" aluminium, but you do need to take into account that the bit is going to be sticking out at least a little more than that. Forces on the bit will cause it to deflect and may cause chatter. I would recommend leaving approximately 0.02" of stock (cut it oversize) for a final finishing path and restricting depth of cut to approx 0.02". Alex.
Thought I would follow up on the Z axis let you know I have it working sort of. I did the factory reset and had to do the custom machine set as there is not a 1510 work bee anymore (it is now obsolete). Had to reset zero settings and home settings. Z axis zero is now the table level setting any positive number above the table setting is the cutting option until the bit is lifted off the part. Completely backwards to what I was use to cutting at. It is working though. Been under the weather for the last few days so I am happy the Z axis is working.
